Fanuc look ahead

[PAnderson]

7 minutes ago, crazy^millman said:

Some customers are never happy. Can be the best program in the world and still complaining. Heard compliant after complaint about a project as it was running. Not efficient I didn't take the age of the machine and how slow it is into account and other things. Then we get the finishing stage and over almost 50" part is within .002" top to bottom. Other places no worse that .0016. Similar easier and smaller part they were seeing as much as .03" deviation. I have to break out the book on what specific parameters effect what. Do you have the Fanuc 5 Axis Help PDF from Europe? There is also a Power Point I found that has good information on this.

Here is a link to both and I offer them freely and make no claim about the authenticity or accuracy of information. In other words use at your own risk.

Fanuc 5 Axis Machining PP

Fanuc 5 Axis Help

 

Yes, I have those. What I don't have is info for tuning the Accell/Decel parameters for 3 axis as well as 5 axis. This is our biggest issue at the moment on some machines. Not all, only a few here and there. But every time it comes up it sheds a bad light on us. And of course, no matter what, some people won't listen on how to use AICC properly. they still program with a .0002" tolerance on everything and I struggle to explain that programming plays as big a role in success as the machine performance does. I had one customer complain that the machine was really jerky, cutting off sharp corners, etc. Sent me the program he was using and they had turned off G5.1 altogether and using a 150IPM feedrate. He said his programmer told him it wasn't needed and the machine should run well without it. We had to send a tech out to show them why it was absolutely needed. Modern machines are tuned with AICC in mind. If you don't use it, you will not get good results.

I would like solid info on Accell/Decel parameters. At least I could see the parameters and know whether it's the parameters or possibly the way they are programming. Our stock 3 axis comes with AICC but only 40 block look ahead. Not good for surface machining. Our 5 axis comes standard with AICC2 and 400 block look ahead. I tell people to spring for the 600 block look ahead. Fanuc tells us it's up to the MTB and won't give me any real guidance on proper Accell/Decel. So, this is probably the one thing I am stuck on.

Thanks for the time and the replies.

Paul

[crazy^millman]

2 hours ago, PAnderson said:

Yes, I have those. What I don't have is info for tuning the Accell/Decel parameters for 3 axis as well as 5 axis. This is our biggest issue at the moment on some machines. Not all, only a few here and there. But every time it comes up it sheds a bad light on us. And of course, no matter what, some people won't listen on how to use AICC properly. they still program with a .0002" tolerance on everything and I struggle to explain that programming plays as big a role in success as the machine performance does. I had one customer complain that the machine was really jerky, cutting off sharp corners, etc. Sent me the program he was using and they had turned off G5.1 altogether and using a 150IPM feedrate. He said his programmer told him it wasn't needed and the machine should run well without it. We had to send a tech out to show them why it was absolutely needed. Modern machines are tuned with AICC in mind. If you don't use it, you will not get good results.

I would like solid info on Accell/Decel parameters. At least I could see the parameters and know whether it's the parameters or possibly the way they are programming. Our stock 3 axis comes with AICC but only 40 block look ahead. Not good for surface machining. Our 5 axis comes standard with AICC2 and 400 block look ahead. I tell people to spring for the 600 block look ahead. Fanuc tells us it's up to the MTB and won't give me any real guidance on proper Accell/Decel. So, this is probably the one thing I am stuck on.

Thanks for the time and the replies.

Paul

In today's age anything less than 600 look ahead is not thinking. Sales always pushing the sale and not the need. Drilling holes all day long okay no need for 600 look ahead, but everything else we are doing today this should just be a must. I tell any customer pay me know or pay me later when it comes to options. Get all the bells and whistles. They are there for a reason and cheaping out on this is just asking for trouble.

Need to talk your boss into sending you to Fanuc classes so you can ask these very questions and then come back and share them with us.

[cncappsjames]

Here's where things get a little confusing for those outside the business. Some builders use the standard set of AICC parameters and other builders use a different group of parameters for servo tuning. "Most" use the standard group or standard plus R (G05.1Q1 R0 through G05.1Q1 R10). Matsuura uses those plus about 75 more. Makes for interesting testing for sure. Thankfully, they come from the factory in good shape. All but the most cycle time conscious are pretty happy with the end result. Some will point out some inefficiency somewhere, and it costs an extra second... yet the machine sits idle for 50% of the day...  

Fortunately, over the years I've learned where I can shave time and still maintain the integrity of the machine. That's the key. A group of us was discussing velocity and machining and the effects high G acc/dec on the life of the machine tool, life of the sheet metal, etc... It was a fun discussion. If you want to sacrifice accuracy and machine lifespan, we can do a lot.

We come standard with 600 and go to 1,000 for certain applications. Anymore, with the types of toolpaths CAM systems are generating, 600 is really BARE MINIMUM ON A 5-Axis. Think about it, on a finishing path, you're going to want between 200µm and 300µm point spacing, and a tool path tolerance between 20µm and 30µm. That's A LOT of points along a 25mm stretch, you need to give the control some room to breathe. IMHO of course.